This example illustrates the sensitivity of the shell elements in
Abaqus
to skew distortion when they are used as thin plates.
An analytical series solution to the boundary
value problem is available in Morley (1963), and an identical evaluation of
elements in numerous other commercial codes is presented by Robinson (1985).
The geometry of the plate is shown in
Figure 1,
Figure 2,
and
Figure 3.
The analysis is performed for five different values of the skew angle,
:
90°, 80°, 60°, 40°, and 30°. Three meshes (4 × 4, 8 × 8, and 14 × 14) are used
for each skew angle in the
Abaqus/Standard
analysis. In the
Abaqus/Explicit
analysis 4 × 4, 8 × 8, and 14 × 14 meshes are used for each skew angle with the
quadrilateral elements and 2 × 2 × 4, 4 × 4 × 4, and 8 × 8 × 4 meshes are used
for each skew angle with the triangular elements.
The plate is 10 mm thick. All sides are 1.0 m long. The length/thickness
ratio is, thus, 100/1 so that the plate is thin in the sense that transverse
shear deformation should not be significant. Young's modulus is 30 MPa, and
Poisson's ratio is 0.3. The plate is loaded by a uniform pressure of 1.0 ×
10−6 MPa applied over the entire surface. The edges of the plate are
all simply supported.
The pressure is applied as a step function in the
Abaqus/Explicit
analysis. Viscous pressure loading is applied to the structure to damp out
dynamic effects. The time period for the step and the viscous pressure are
chosen to obtain an optimal static solution.
Results and discussion
Three response quantities are presented: the vertical displacement in the
center of the plate, ,
and the maximum and minimum bending moments per unit length at the center of
the plate, defined as
where
The bending moment values ,
and
are obtained from the average nodal values obtained by requesting element
output to the data file in the
Abaqus/Standard
analysis. These values are calculated by extrapolation from the integration
point values in the elements, followed by averaging of these values over all
elements attached to the node. They are, therefore, less accurate than the
values at the integration points. In the
Abaqus/Explicit
analysis the bending moment values are obtained from an average of the
integration point values for all elements that share the node at the center of
the plate.
Abaqus/Standard
results
The results for the 3-node triangular shells, S3R and STRI3, are given in
Table 1
and
Table 2,
respectively. These elements give reasonable results for all skew angles with
all but the coarsest mesh used (4 × 4 elements).
The results for the 6-node triangular shell STRI65 are given in
Table 3.
This element gives reasonable results for all the skew angles with the various
mesh discretizations, with the exception of the coarsest mesh used.
The results for the 4-node quadrilateral shells are presented in
Table 4
(S4R5),
Table 5
(S4R), and
Table 6
(S4). The performance of these elements in this case is rather
similar to that of the triangular elements.
The results for element types S8R5 and S9R5, presented in
Table 7,
are essentially identical to each other. These second-order elements are more
sensitive to the distortion in this problem than the first-order elements. For
80° and 90° angles they give slightly more accurate displacement values than S4R5; but at more severe angles their performance deteriorates
noticeably, particularly in the prediction of the minimum moment at the center
of the plate. It is possible that this is caused by the extrapolation and
averaging technique used to obtain nodal values of bending moments rather than
an intrinsic sensitivity of the elements to this type of distortion.
The results for element type S8R are given in
Table 8.
Except with the finest mesh used, this element generally shows greater loss of
accuracy as the plate is skewed than any of the other elements.
The results for the continuum shell elements SC6R and SC8R are presented in
Table 9
and
Table 10.
The performance of these elements is similar to that of the S3R and S4R shell elements.
Abaqus/Explicit
results
The explicit dynamic analysis is run until a steady, static solution is
obtained.
Figure 4
shows an energy balance plot for the 14 × 14 mesh with a skew angle of 40°. It
can be seen that inertia effects have died away.
The results for the 3-node triangular shell, S3R, are given in
Table 11.
These elements exhibit stiff response for the coarsest mesh used (2 × 2 × 4
elements) but converge to the correct answer as the mesh density is increased.
The results for the 4-node quadrilateral shells, S4R and S4RS, are presented in
Table 12
and
Table 13,
respectively. For all but the 40° and 30° skew angles, the S4R elements give reasonable answers for the coarsest mesh used. As
the mesh density is increased, the elements converge to the analytical
solutions for all skew angles.
The results for the continuum shell element SC8R are presented in
Table 14.
The performance of this element is similar to that of the S4R shell element.
General remarks
Abaqus
gives a warning when quadrilateral elements are defined with skew distortions
larger than 45°. The results in this case indicate that, with the possible
exception of element type S8R, the elements can provide quite accurate results with reasonable
meshes even with large skew distortions. Nevertheless it is also clear that the
analyst should attempt to design meshes to avoid distortion of the elements in
any region where there are large strain gradients.
Comparison of the results reported here with the evaluations given by
Robinson (1985) indicate that the elements in
Abaqus
are among the most accurate and least sensitive to skew angle.
Parametric study using a parametric study script
The skew sensitivity investigation discussed in this example can be
performed conveniently as a parametric study using the Python scripting
capabilities offered in
Abaqus.
As an example we perform a parametric study in
Abaqus/Standard
in which 15 analyses are automatically executed; these analyses correspond to
combinations of five different values of the skew angle
(:
90°, 80°, 60°, 40°, and 30°) for three different element types (S8R, S4R, and S4). We also perform a parametric study in
Abaqus/Explicit
in which 12 analyses are executed automatically; these analyses correspond to
combinations of three different values of the skew angle
(:
90°, 60°, and 30°), two different element types (S4R and S4RS), and two mesh discretizations (4 × 4 and 8 × 8 elements).
skewshell_parametric.inp shows
the parametrized template input data used to generate the parametric variations
of the
Abaqus/Standard
parametric study. The parametric study script file (skewshell_parametric.psf) is
used to perform the parametric study. The vertical displacement in the center
of the plate is reported in the following table for each of the analyses of the
parametric study:
These results match the corresponding results found in
Table 5
to
Table 8.
skew_discr.inp shows the
parametrized template input data used to generate the parametric variations for
the
Abaqus/Explicit
parametric study. The parametric study script file (skew_discr.psf) is used to
perform the parametric study. The vertical displacement at the center of the
plate is reported in the following table for each analysis of the parametric
study:
Morley, L.S.D., Skew
Plates and
Structures, Pergamon
Press, London, 1963.
Robinson, J., “An
Evaluation of Skew Sensitivity of Thirty-Three Plate Bending Elements in
Nineteen FEM Systems,” paper presented at the
Finite Element Standards Forum at the AIAA/ASME/ASCE/AHS 26th Structures,
Structural Dynamics, and Materials
Conference, April
1985.
Figure 1. Simply supported skew plate with uniform distributed load. A 4 × 4
mesh for the complete plate of quadrilateral elements is shown. The
corresponding mesh of triangular elements is shown by the dotted line. Figure 2. 4 × 4 mesh for the complete plate of quadrilateral elements. Figure 3. 2 × 2 × 4 mesh for the complete plate of triangular elements. Figure 4. Energy balance for 14 × 14 mesh at 40° (Abaqus/Explicit
analysis).
